Reaming holes in aluminum (feeds/speeds)

ProjectZero · Aug 29, 2017

Hi guys,

Trying to get my reaming feeds and speeds right in aluminum...still relatively new to CNC. I'm used to using FSWizard and just trusting its numbers but for reaming I think I need to dig a little deeper and make sure I'm doing it right. I've tried reaming some holes before and they're bell like - definitely flared a bit in the beginning.

Right now I'm using a small 1/16th under reamer. .0624. I'm predrilling it using a .052 drill bit (#55). Now I usually trust FSWizard for flat end mill and twist drill feeds/speeds. For the predrill it tells me to use 10000 RPM (max of my machine) and 13 in/min feed rate. I've heard the rule of thumb is twice the feed and half the RPM. So for my .0624 reamer should I go 4500 RPM and 26 in/min feed rate? Does that sound about right?

Another question (more CAM) should I enter 26 in/min for both the Cutting Feedrate and the Plunge Feedrate?

I've emailed the manufacturer asking for recommended SFM for my .0624 reamer and am waiting to hear back. Thank you for your advice!

gkoenig · Aug 29, 2017

That's a big bite for a reamer when you're getting to holes that small. The first thing I would do is step up to a larger drill, either a 1.5mm or a #54. The bellmouthing sounds like the initial chip forming at the start of the reaming, as the pressure rises to start pushing the chips up the flute.

Shawnrs · Aug 29, 2017

Open up your drill like Gkoenig said but slow down your reamer to S2000-1500 and feed between F5.0 - F10.0 as a starting point and work your way up. Make sure your reamer is not sticking too far out when reaming the holes. You can also use a G85 boring cycle where it feeds in and feeds out or use a drilling cycle G81 where it feeds in and rapids out.

ProjectZero · Sep 27, 2017

Shawnrs said:
Open up your drill like Gkoenig said but slow down your reamer to S2000-1500 and feed between F5.0 - F10.0 as a starting point and work your way up. Make sure your reamer is not sticking too far out when reaming the holes. You can also use a G85 boring cycle where it feeds in and feeds out or use a drilling cycle G81 where it feeds in and rapids out.

Hey sorry to necro this topic but thanks for the info guys...so the S2000 and F5 worked pretty well. My only question is, how do you calculate that?? If I look up charts for reaming AL they give me an SFM of about 150 and IPT of about .004 so I calculate something wild like 9000 RPM and 37 feed rate. And FSWizard gives me 9000 RPM and 23 in/min feed rate. Both of which are clearly wrong.

So how do I properly calculate feed rate? I can't post on Practical Machinist every time

ProjectZero · Sep 27, 2017

Shawnrs said:
Open up your drill like Gkoenig said but slow down your reamer to S2000-1500 and feed between F5.0 - F10.0 as a starting point and work your way up. Make sure your reamer is not sticking too far out when reaming the holes. You can also use a G85 boring cycle where it feeds in and feeds out or use a drilling cycle G81 where it feeds in and rapids out.

Hey sorry to necro this topic but thanks for the info guys...so the S2000 and F5 worked pretty well. My only question is, how do you calculate that?? If I look up charts for reaming AL they give me an SFM of about 150 and IPT of about .004 so I calculate something wild like 9000 RPM and 37 feed rate. And FSWizard gives me 9000 RPM and 23 in/min feed rate. Both of which are clearly wrong.

So how do I properly calculate feed rate? I can't post on Practical Machinist every time

G00 Proto · Sep 27, 2017

ProjectZero said:
Hey sorry to necro this topic but thanks for the info guys...so the S2000 and F5 worked pretty well. My only question is, how do you calculate that?? If I look up charts for reaming AL they give me an SFM of about 150 and IPT of about .004 so I calculate something wild like 9000 RPM and 37 feed rate. And FSWizard gives me 9000 RPM and 23 in/min feed rate. Both of which are clearly wrong.

So how do I properly calculate feed rate? I can't post on Practical Machinist every time

You don't. You try a bunch of shit that doesn't work and then settle on some numbers that work for YOU. You have numbers that work for a 1/16" Reamer, then you scale those numbers for an 1/8" and then a quarter... after about 20 years you have numbers that work for just about everything. Reamers are a black art... we like to say twice the feed and half the speed as the drill, but that presumes you're drilling correctly

Then you throw lubrication into the equation and all bets are off. I can make a reamed hole drift .0005 or more by what cutting oil I use. I wish there was simple answers, but the only one is to keep notes on what worked and what didn't. If I would have done that 25 years ago, I wouldn't continually repeat the same mistakes.

Mtndew · Sep 28, 2017

G00 Proto said:
Reamers are a black art..

Ain't that the truth!

cpifer3 · Sep 28, 2017

drilling 3-5% smaller than the reamer works good for me, but like others have said, so many variables.

onecut · Sep 28, 2017

You get to know your machine get a notepad and note succesful results on various materials note size of reamer and drill used and then you dont need to calculate or rely on wizards or black magic.Using inch reamer on stainless you have done it before succesfully you know how long it took and have the speed/feed away you go even then because of variations in same materials you may need to tweak.Thats far too much you were leaving in the hole for the reamer,leaving less/more material in a hole you can get the same reamer to cut different sizes with trial and error.Thats why a previous reference take a few minutes and cant do you any harm for the next batch

rainman · Sep 28, 2017

G00 Proto said:
Reamers are a black art...

That's for sure! Murphy likes reamers. If you want one to cut exactly what it mics, it will go over. If you want it to go a few tenths over, it cuts right on size!

gregormarwick · Sep 28, 2017

G00 Proto said:
Reamers are a black art

Yep, and because of that boring tools outnumber reamers 10 to 1 here.

I have been fucked over by reamers enough times that I will go to great lengths to avoid using them.

G00 Proto · Sep 28, 2017

gregormarwick said:
Yep, and because of that boring tools outnumber reamers 10 to 1 here.

I have been fucked over by reamers enough times that I will go to great lengths to avoid using them.

Ain't that the truth. Seems like when I started out, reamers were the gospel for making an accurate sized hole and circle milling a hole was considered a crude approximation. CNC machines weren't as good and quite frankly we didn't use CMMs and Deltronics gage pins as much. Once the QC got better (and CNCs got better), I started to drift away from reamers and more towards circle milling accurate holes (generally above .125" for me). I know deep down, that a circle milled hole is not round, but I also know that I can set cutter comp .001" big on the first part, and sneak up on it with gage pins to get exactly the fit I desire.

I've often thought that some high quality, miniature boring tools might be a sweet way to make accurate holes. Round, good location accuracy and adjustable. How small can you go?

mhajicek · Sep 28, 2017

G00 Proto said:
I've often thought that some high quality, miniature boring tools might be a sweet way to make accurate holes. Round, good location accuracy and adjustable. How small can you go?

I think aspect ratio is more of a limiting factor for boring bars than size, to a point. You can get some pretty small solid carbide boring bars from PH Horn and the like, but they won't go very deep.

gregormarwick · Sep 28, 2017

G00 Proto said:
How small can you go?

Our 50mm d'andrea heads can take 16mm shank bars, and I have a couple of sandvik corocut holders that I've shortened to fit in them. So for shallow holes, down to 0.3mm in theory, and 2μm adjustment.

Smallest I have actually gone with those is 4mm.

For deep holes, the D'andrea heads go down to 14.5mm. The smallest one I have is 22mm. Also 2μm adjustment. Really nice tools.

ProjectZero · Sep 28, 2017

You don't. You try a bunch of shit that doesn't work and then settle on some numbers that work for YOU. You have numbers that work for a 1/16" Reamer, then you scale those numbers for an 1/8" and then a quarter... after about 20 years you have numbers that work for just about everything. Reamers are a black art... we like to say twice the feed and half the speed as the drill, but that presumes you're drilling correctly Then you throw lubrication into the equation and all bets are off. I can make a reamed hole drift .0005 or more by what cutting oil I use. I wish there was simple answers, but the only one is to keep notes on what worked and what didn't. If I would have done that 25 years ago, I wouldn't continually repeat the same mistakes.

Damn you know I had a feeling this was the idea, even though I hoped it wasn't. When you say you scale those numbers, is there some sort of scaling factor? Like if the S2000 F5 works well for a 1/16 reamer, do I double it for a 1/8" reamer?

G00 Proto said:
Ain't that the truth. Seems like when I started out, reamers were the gospel for making an accurate sized hole and circle milling a hole was considered a crude approximation. CNC machines weren't as good and quite frankly we didn't use CMMs and Deltronics gage pins as much. Once the QC got better (and CNCs got better), I started to drift away from reamers and more towards circle milling accurate holes (generally above .125" for me). I know deep down, that a circle milled hole is not round, but I also know that I can set cutter comp .001" big on the first part, and sneak up on it with gage pins to get exactly the fit I desire.

I've often thought that some high quality, miniature boring tools might be a sweet way to make accurate holes. Round, good location accuracy and adjustable. How small can you go?

Man. Tell me more. Unfortunately I've got this 2005 Fadal VMC and I don't have the fancy tools of my old mill. I'm not an expert, I'm a mechanical engineer who was the only one who had done milling at all before so guess who's in charge of it

? I haven't figured out how to do cutter comp on this machine. So I'm plugging in the nominal end mill size and hoping it's not too worn. So I know my interpolated holes aren't very close. I also don't have a CMM to bore out some test holes and figure out *exactly* how close to nominal they are.

So I'm using reamers because it seems to be the best way for me to get precise holes with my limited CNC knowledge. I might need to look into boring bars though? I'm not familiar with them.

allloutmx · Sep 28, 2017

There is a book called Machining Data Handbook. About the only thing I use it for is reamers. HSMadvisor and mfg specs for most everything else I do. There are a zillion ways you can process a hole for reaming. Most times I drill-then interpolate leaving minimal material for the reamer while using as much flute as possible so that the hole is as taper free as possible and dead on location then chase with a reamer if you must.

onecut · Sep 30, 2017

A Tip is to drill/bore the hole then ream look in your data hand book for stock allowance.Doing it this way your reamer will not follow an off line toolpath caused by any drill error so you should end up with a round true hole hopefully in tolerance.Especially applies to deep holes where the drill can drift off line and the reamer will follow

gregormarwick · Sep 30, 2017

onecut said:
hopefully in tolerance

"hopefully" is the key word here. Every bloody thing about reamers boils down to keeping your fingers crossed and hoping it works.

If I've got a part that I'm 30 hours into and two grand in material and the last op is a little hole with any combination of remotely tight position/diameter/roundness/straightness/surface finish tolerances, then you can be absolutely certain that I'm not putting a reamer anywhere near it.

litlerob1 · Sep 30, 2017

gregormarwick said:
"hopefully" is the key word here. Every bloody thing about reamers boils down to keeping your fingers crossed and hoping it works.

If I've got a part that I'm 30 hours into and two grand in material and the last op is a little hole with any combination of remotely tight position/diameter/roundness/straightness/surface finish tolerances, then you can be absolutely certain that I'm not putting a reamer anywhere near it.

Reamers are really a last resort for me. I'll send it to the Fab shop and have them try to Air-Arc a hole before I run a reamer. :bawling:

Once I get below about 3/16" I can Drill very round, very straight, fine finished holes, Reamer can suck it.

R

Corym · Oct 2, 2017

I use these charts to good effect

http://www.rockrivertool.com/documents/reaming-speeds-and-feeds.pdf

http://www.rockrivertool.com/documents/pre-ream-drill-size-chart.pdf

Reaming holes in aluminum (feeds/speeds)

Aluminum

Titanium

Stainless

Aluminum

Aluminum

Hot Rolled

Diamond

Cast Iron

Hot Rolled

Cast Iron

Diamond

Hot Rolled

Diamond

Diamond

Aluminum

Titanium

Hot Rolled

Diamond

Diamond

Cast Iron

Similar threads